How Aluminum Parts Formed by CNC Reach ±0.005 mm
This page explains what actually happens when aluminum parts formed on a machining center, where the limits sit, and which geometry tells you to pick 3-axis, 5-axis, or turning. It is written for design engineers and buyers who have to sign off a drawing before the first chip is cut.
Key takeaways
What Happens at the Tool Tip
Aluminum parts formed on a CNC mill start as a solid block that gets reduced by a rotating cutter. The edge of that cutter shears metal away in a narrow band of plastic deformation. Everything that follows, the surface finish, the tolerance that holds, the burr you have to remove, comes out of how that band behaves.
Aluminum 6061-T6 needs about 0.5 to 1.2 kW of spindle power per cm³/s of material removed. Compare that to 304 stainless, which needs roughly three times more. That gap is why aluminum parts can be cut fast, with deep axial passes and high feed rates, on machines that would chatter on steel.
The tool tip does not stay sharp. Built-up edge forms when aluminum welds to the cutting edge under heat and pressure, then breaks off and takes a small piece of the tool with it. The result is a torn surface and a dimension that drifts. High rake angles, polished flutes, and cutting fluid aimed directly at the tip keep that weld from forming.
Chip evacuation is the quiet constraint. Aluminum chips are soft and bulky. In a deep pocket, they pack into the flute and recut, which doubles the heat and triples the load on the edge. If you see a pocket that is deeper than four times its width, the machinist will slow down, not because the material is hard, but because the chips have nowhere to go.
- 1Rake angle12–20° positive for 6061, lower for 7075 to keep the edge from chipping.
- 2Surface speed300–600 m/min with carbide, higher with PCD on long runs.
- 3CoolantFlood or through-spindle. Air blast alone tears the finish on deep cuts.
Why Heat Sets the Tolerance Floor
Aluminum expands at roughly 23 × 10⁻⁶ per °C. A 300 mm part that warms by 5 °C during roughing grows about 0.035 mm. That is seven times the ±0.005 mm tolerance. The number is not a warning about sloppy work; it is the reason finishing passes happen on a cooled part, not a hot one.
In practice, the machinist roughs the part, lets it sit, then takes the finishing cut after the stock returns to room temperature. On a 4,000 mm part, that waiting period can be longer than the cutting time. Shops that skip it ship parts that measure right on the machine and wrong in the inspection room.
Thin walls make this worse because they have less mass to absorb heat and they move when the surrounding material is removed. A 1 mm wall on a 100 mm tall rib can bow 0.05 mm from residual stress alone, before any thermal effect. Stress relief, either by pre-machining or by choosing a tempered temper like T6 or T651, is the standard fix.
The practical takeaway for a drawing is simple. Tight tolerances on long thin aluminum parts are not a machining problem. They are an inspection problem. You need to specify the temperature at which the part is measured, or accept that the number will drift with the shop floor.
How Alloy Choice Changes the Cut
6061-T6 is the default for aluminum parts formed by CNC. It machines clean, welds well, anodizes to a uniform color, and holds ±0.005 mm without drama. If your drawing does not name an alloy, this is what a shop will quote.
2024 and 7075 are stronger but less forgiving. 7075-T6 reaches about 570 MPa yield, close to mild steel, and it work-hardens at the cut. A dull tool will chip the edge instead of shearing the chip. Machinists compensate with lower rake angles, lighter feeds, and more frequent tool changes. Expect a higher price per part, not because the material costs more, but because the tooling does.
5052 and 5083 are marine grades. They form well and resist corrosion, but they are gummy on a mill and tend to smear rather than cut. If a part needs both machining and bending, 5052 is often better than 6061 because it bends without cracking at a tighter radius.
ADC12 is a die casting alloy, not a wrought one. It shows up when a design starts as a casting and later needs machined features. It cuts easily but contains porosity, so a sealing face or a press-fit bore may need a local insert or a change to the casting gate.
- 16061-T6General purpose. Best finish-to-cost ratio for machined parts.
- 27075-T6High strength. Use for aerospace brackets and stressed fittings.
- 35052 / 5083Formable and corrosion resistant. Good for enclosures and panels.
- 42024-T4Fatigue resistant. Common in aerospace, harder to anodize evenly.
Why Setup Count Decides Final Accuracy
Every time a part leaves a fixture and comes back, the datum shifts. A 3-axis machine working five faces needs three or four setups. Each re-clamp adds 0.01 to 0.03 mm of position error, depending on the fixture and the operator. That error is random, so it does not cancel out.
A 5-axis machine holds the part in one vise and rotates the table. Hole-to-hole position across five faces stays inside a single setup error, often 0.005 mm or better. For parts with bores on multiple faces that must align, this is the deciding factor, not the surface finish.
The trade-off is tool reach. A 5-axis spindle tilts, but the tool still has to clear the fixture and the part. Deep cavities with a 5-sided opening may need a long tool that deflects under load. In that case, two 3-axis setups with a purpose-built fixture can hold a tighter bore than one 5-axis setup with a flexible tool.
There is also a time cost. A 5-axis setup takes longer to program and prove out. For a one-off bracket with two holes, 3-axis is faster end to end. For a 200-part run with bores on four faces, 5-axis wins on both accuracy and cycle time.
How the Number Is Actually Verified
A tolerance is a claim about a measurement. If the drawing says ±0.005 mm and the inspection report uses a caliper, the claim is not supported. A caliper reads to 0.02 mm on a good day, and the operator's hand adds more error than the part.
For aluminum parts formed to tight limits, the verification chain runs from a coordinate measuring machine for position and form, to a micrometer for outside dimensions, to a bore gauge or an air gauge for internal diameters. Surface finish gets checked with a portable profilometer at the same spots the drawing calls out.
Temperature matters here too. A part measured at 28 °C on the shop floor reads differently than the same part at 20 °C in a metrology room. For a 300 mm aluminum part, that 8 °C difference is about 0.055 mm. Shops that care about the number either control the room or record the temperature on the report.
GreatLight inspects every part before shipment and keeps raw material, in-process, and final inspection records. Reports go out on request. The point is not the paperwork. It is that a tolerance you cannot measure is a tolerance you cannot hold.
- 1CMMPosition, true position, form. The reference for GD&T callouts.
- 2MicrometerOutside dimensions down to 0.001 mm resolution.
- 3ProfilometerRa and Rz at the specific surfaces named on the drawing.
- 4Air gaugeFast, repeatable bore checks on high-volume runs.
Which Process Fits Which Feature
Use the feature, not the part name, to pick the process.
| Feature | Best process | Why | Watch out for |
|---|---|---|---|
| Open pocket, 3 sides | 3-axis milling | One setup, tool reaches from above | Deep pockets need chip clearance |
| Holes on 4 faces | 5-axis or 2 setups | Avoids re-clamp stack-up | 5-axis quoting needs the model |
| Ø20 mm shaft, 0.01 mm round | CNC turning | Work rotates, tool stays still | Long shafts need a steady rest |
| Thin rib under 1.5 mm | 3-axis with stress relief | Light finishing passes control bow | Measure after cooling, not hot |
| Undercut or 5-sided cavity | 5-axis simultaneous | Tool angles into the cut | Short tools only, check reach |
| M2 thread, 8 mm deep | Thread milling | Tap breaks before thread fails | Add 30 seconds per hole |
| 400 mm flat face, Ra 0.8 | 3-axis with fly cutter | Single sweep, no step marks | Check machine travel first |
Tolerance and Finish by Operation
| Operation | Typical tolerance | Typical finish | Best for |
|---|---|---|---|
| 3-axis milling | ±0.01 mm | Ra 1.6–3.2 μm | Open pockets, flat faces, plates |
| 5-axis milling | ±0.005 mm | Ra 0.8–1.6 μm | Multi-face bores, contoured pockets |
| CNC turning | ±0.005 mm | Ra 0.8–1.6 μm | Shafts, bushings, threaded bosses |
| Mill-turn | ±0.005 mm | Ra 0.8–1.6 μm | Parts with turning and milling in one |
| Fine boring | ±0.005 mm | Ra 0.2–0.8 μm | Bearing bores, sealing faces |
| Thread milling | Class 6H | Ra 1.6 μm | Threads below M3 or in thin walls |
The Choice in One Line
If the bores must align across several faces, pay for one 5-axis setup. If the part is flat and open, 3-axis gets you the same tolerance for less money. Never specify ±0.005 mm on a feature you cannot measure.
Questions Engineers Ask
What is the thinnest wall I can machine in aluminum?
A 0.8 mm wall is practical on a 6061 part with a stable shape and light finishing passes. Below that, the wall deflects under cutting pressure and vibrates, which shows up as chatter marks and a dimension that moves.
If the design needs a 0.5 mm wall, plan for a support structure or a change to a formed or cast process. Machining it is possible but the yield drops and the cost per good part rises fast.
Can you hold ±0.005 mm on a 500 mm long aluminum part?
Yes, on features near the datums and after the part has cooled. Over the full 500 mm length, thermal expansion and residual stress make the number harder to hold than on a small part.
The usual approach is to machine the critical features in one setup, measure at 20 °C, and accept a slightly wider tolerance on the non-critical length. Call it out on the drawing so the shop can plan.
Why does my anodized part measure differently than the bare part?
Anodizing grows the surface by roughly half the oxide thickness. Type II clear adds about 5 to 10 μm per side, so a bore shrinks and an outside dimension grows. If the drawing tolerance is tight, mask the feature or specify the dimension after coating.
Hardcoat adds more, often 25 to 50 μm, and it is not uniform on sharp edges. For press fits, machine to the pre-coat size and tell the finisher which surfaces matter.
When should I use thread milling instead of tapping?
Below M3, or in any thread where the wall around the hole is thin, thread milling is safer. The tool cuts with a helical path and never bottoms out under torque, so it does not snap inside the part.
It also lets you cut a thread in a hardened or gummy alloy where a tap would bind. The cost is cycle time, roughly 20 to 40 seconds per hole depending on depth.
Does 5-axis machining always give a better finish?
No. Finish comes from tool geometry, feed per tooth, and rigidity, not from the number of axes. A 5-axis machine with a long tool in a deep pocket can leave a worse finish than a 3-axis machine with a short, stiff tool.
Use 5-axis for access and setup reduction. Use the right tool and the right stepover for finish.
What do you need to quote an aluminum part?
A 3D model in STEP or IGES, a 2D drawing with tolerances and finish callouts, the alloy, the quantity, and any surface treatment. If the drawing is missing, we can work from the model and flag the features that need a tolerance.
Quotation and a DFM analysis come back within 12 hours. Production can start within 24 hours after the order is confirmed.
Send the Drawing, Get a Real Number
Upload your model and drawing. We review the geometry against our 127 CNC machines, flag what will not hold, and quote within 12 hours.
12-hour quote100% inspectionNo minimum orderNDA on request
More from the shop floor
We publish setup notes, tooling trials and inspection data from the factory floor.
